# Using ID's on sheetmetal parts

My brake operators prefer to use ALL inside dimensions when forming a part with no specified radii. I can't figure out how to get solidworks
to recognize this. The closest I've come to achieving my goal is to specify a .0001 default radius, and a k factor of 0. I run into problems with this on some thicker parts when solidworks HAS to put a bend radius in it. My flat layouts always come up with bogus dimensions (at least according to the brake operators) and creates some major headaches for me, and them. Is there a bend table I should be using for A36 ms plate? Am I missing something? I haven't seen any other threads addressing this problem.
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Chad, Unless you are using some really strange A36, then you have to put in a realistic bend factor. You should also specify a radius, unless consistent and repeatable parts are not needed. A 0.4 k factor would be a good place to start. Your specified bend radius is going to depend on what size die they are using, assuming they are air bending the part. 1.25*thickness is a good place to start. Once you get your k-factor dialed in and the radius correct, the flat pattern should be correct. I have a excel spreadsheet with different material and bend radii that I could send to you if needed. Brian

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I'm a bit confused as all bending operations will involve a radius of some size, unless you get into coining, which I don't think is your issue. My suggestion is to determine what the K-factor is of the current operations and then use those values. To test it, shear out a piece of the material, measure it accurately, bend it, and the measure it again. That way you will know what the bending process is producing.
WT

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I should have been more specific, sorry about that. We have a 500 ton Cincinatti hydraulic press brake with v bottom dies. The issues I speak of for example, when I form a Channel shape out of lets say .25 material thickness the brake operators want only Inside dimensions, i.e. 5" flange with 2" legs (inside dimensions) the brake operators want exactly 9" of material, no more, no less, and this is the way we've always done it, and it serves us well. However, solidworks wants to make it a little more or a little less depending on bend radii and bend allowance. I hope this helps clear some things up...
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It's just a matter of picking the correct bend radius and k-factor. For 1/4" material, try k-factor = .4, inside radius = .366

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Awesome Brian, that worked great! Is there a bend table allowance I should be using to get these figures on a consistent basis? Or is is pretty much a guessing game?
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Use Bend Deduction and set it to 0. This will produce the results you are looking for.
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Dave I tried this, and yes, it does work, sometimes, with a default radius to .0001 or somewhere around there, however it has a hard time bending and unbending some of the thicker metals that require a larger radius.
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Please send me one of the parts you are having a problem with. dherb_ma_n_@ho_tmail.com ^^REMOVE UNDERSCORES^^
I'm guessing the issue is related to bend relief or edges intersecting the bend region. I double checked by creating a sheet metal angle with 2"x2" legs and setting Bend Deduction to 0, then mucking around with the variables.
Material Thickness: .375 IBR: .375 Flat pattern= 4"
Material Thickness: .375 IBR: .0001 Flat pattern= 4"
Material Thickness: .5 IBR: .5 Flat pattern= 4"
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